UG Drafting Associativity 1

[Juhler]

Hi

I am new to this forum, but I have a problem with NX 5.0.

When in drafting, I some times need to redo a measurement who has been associated with another measurement. Deleting it resolves in dotted lines, and no ability to get it back to normal (see picture).

Is there a way to make it complete again with out redoing it? I know I can create measurements without associativity by holding down the ALT key.

/Juhler

 

[JohnRBaker]

In NX we call those 'Dimensions'. What's happened is that the 'Dimension' has become detached from what it was referencing (this can happen for a couple of reason, usually because an edit made and the edge was being referenced no longer exists) and has gone into what's known as the 'retained' state.

You can reattach the 'Dimension' to a desired edge/point by selecting the extension line you wish to reattach, press MB3 and select the 'Edit Associativity...'. Now you can select a new edge/point and the dimension will snap to it. If it remains dashed, then you will need to reattach the other extension line as well using the same workflow as you used on the first extension line.

John R. Baker, P.E.
Product 'Evangelist'
Product Engineering Software
Siemens PLM Software Inc.
Industry Sector
Cypress, CA

http://www.siemens.com/plm

UG/NX Museum:

http://www.plmworld.org/p/cm/ld/fid=209

To an Engineer, the glass is twice as big as it needs to be.

 

[MickyV007]

Associate it with the geometry of your part. Just double click on the dimension, you will get the reattach menu. In your example the 8.0 dimension make it associative with the bottom of your part and with the straight piece where the threaded hole is in.

Best regards,

Michaël.

NX7.5.4.4 + TC Unified 8.3
Win 7 64 bit

 

[Juhler]

Dimensions, that was the word I was looking for.

Thank you for your swift reply, but I cannot seem to get it to work. Regardless of which option I choose under the 'Edit Associativity' it remains dashed. I will keep trying, but I think eventually I will have to get used to pressing the ALT key everytime, when creating a dimension.

/Juhler

 

[MickyV007]

I've added a movie, maybe it explains it a bit more.

Best regards,

Michaël.

NX7.5.4.4 + TC Unified 8.3
Win 7 64 bit

 

[Juhler]

Problem solved by Michael, here is the solution for people with the same problem:

If you use MB3 choose the Origin option in the menu. Then will see a check box Associative, it will not be checked, check it, then pick the geometry and your dimension will be attached to the geometry instead of to the deleted dimension. Now afterwards you also can work with the Edit associativity option...